Foundation Course Part Design - WordPress
AIRBUS UKCATIA V5 Foundation CourseFoundation CoursePart DesignCompiled by: Kevin BurkeApproved by:Authorised by:Date:Date:Kevin BurkeDate: 16/Apr/2003AIRBUS UK Ltd. All rights reserved.DMS42184ANS-UG0300110Page 1 of 90Issue 1
AIRBUS UKCATIA V5 Foundation CourseDocument ControlAmendment ded ByMary HartiganAmendment DetailsANS number added (Airbus NumberingSystem)Page 2 of 90Issue 1
AIRBUS UKCATIA V5 Foundation CourseContentsSession 4 – The Part Design Workbench.4An Introduction to Part Design . 5Accessing the Part Design Workbench . 8Part Design Toolbars and Icons . 9The Sketch Based Features Toolbar. 10Creating Pads. 10Hints and when creating Pads . 16Creating a Pocket . 20Creating a Shaft. 23Creating a rotational Groove . 25Creating a Rib feature . 32Creating a Slot Feature. 34Creating a Stiffener . 35Creating a Loft Feature . 37The Remove Loft Feature . 41Creating Reference Elements Toolbar . 41Create a Point in 3D Space. 41Creating Lines in 3D Space. 44Creating Plane in 3D Space. 46Surface Based Operations Toolbar. 49Creating a Split. 49Thick Surface . 51Boolean Operations Toolbar . 52The Assemble Operation. 52Standard Boolean Operations. 54The Union Trim Operation. 55The Remove Lump Operation. 56Dress-Up Features Toolbar . 57Creating Fillet Features . 57Creating Chamfer Features. 65Creating a Draft Feature. 66Creating a Shell Feature . 70The Thickness Feature . 72Transformation Features Toolbar. 73Standard Transformations . 73Mirror Body. 75Patterns . 76Scaling. 83Part Design Constraints Toolbar . 84Create Constraints using a dialog box. 84Create Constraints by selecting elements. 85Using Compass Manipulation . 86Creating an User Defined Axis System. 89DMS42184ANS-UG0300110Page 3 of 90Issue 1
AIRBUS UKCATIA V5 Foundation CourseSession 4 – The Part Design WorkbenchOn completion of this session the trainee will: Be able to access the Part Design Workbench. Understand the Part Design Toolbars and Icons. Be able to create Sketch and Surface Based Features. Be able to Perform Boolean Operations. Be able to create Dress-Up Transformation Features. Be able to use the Compass Manipulation. Be able to create a User Defined Axis System.DMS42184ANS-UG0300110Page 4 of 90Issue 1
AIRBUS UKCATIA V5 Foundation CourseAn Introduction to Part DesignThe Part Design Workbench is used to create Solid geometry using a Feature basedapproach. In general the features are produced from sketches created in the Sketcherworkbench.The specification tree contains all the features created along with the sketch used todefine them. All the Solid features are contained within a node called a PartBody.They also contain wireframe sketches that are used to create the features. As youcreate features they are added to the tree in order of creation. There may be multiplePartbodies within a CATPart which can be Booleaned together in order to formcomplex solid models. Partbodies can be added to the Specification Tree by selectingBody from the Insert drop down menu when in the Part Design Workbench. ThePartbody can then be renamed by editing its properties.If an existing feature is used in the creation of a new feature i.e. the sketch plane forthe new feature is created on an existing Face of another feature then the new featureis dependent on it. Therefore the existing feature becomes the Parent of the newfeature which is known as the Child. If the Parentfeature is deleted the Child feature will need to beedited and attached to a new parent or in somecases it may be isolated otherwise it to will bedeleted. Prior to deleting a feature you canascertain its dependencies by selecting the nodeon the tree and by using MB3 select Parent/Childon the Contextual Menu. A pop up Parent andChildren window will appear displaying thefeatures dependencies.In the example opposite Pocket.3 is dependent onSketch.2, also EdgeFillet.4 is depend onPocket.3. Therefore if the sketch is deleted thenboth the pocket and fillet features will be deleted.By using MB3 on a selected node in the windowyou can edit the feature to change itsdependencies. Once you have finished click OKor Cancel to closed the window.DMS42184ANS-UG0300110Page 5 of 90Issue 1
AIRBUS UKCATIA V5 Foundation CourseWhen you are modifying or creating sketches or features in the Specification Tree thenode is underlined.If you select another node on the tree and byusing MB3 and selecting Define in Work Objecton the Contextual menu you can step back inhistory and display the solid model at earlierstage of is evolution and you can then proceed toedit the command.In this case before the Holes and Fillets werecreated.DMS42184ANS-UG0300110Page 6 of 90Issue 1
AIRBUS UKCATIA V5 Foundation CourseIf you select a Partbody and Define it as the Work Object then it is possible to Scanthrough the entire history of the Partbody by selecting Scan or Define in WorkObject option on the Edit drop down menu. A Scan panel will appear and by usingthe arrow button you can step through the history.Exit ScanmodePreviousNextFirstLastIt is best to select the the First button to begin at the start of history. The Next buttonwill move forward one command and the Previous button will step back onecommand. The Last button jumps to the end of history. Finally the square button exitsScan mode.SpecificationTreeFeature basedSolidPartBodyNodeSurface basedFeaturesSolid Page 7 of 90Issue 1
AIRBUS UKCATIA V5 Foundation CourseAccessing the Part Design WorkbenchTo access the Part Design workbench you can either Select Start MechanicalDesign Part Design from the Start drop down menuAgain if a CATPart is not active you will be prompted to create a new part by theappearance of the Part name panel.DMS42184ANS-UG0300110Page 8 of 90Issue 1
AIRBUS UKCATIA V5 Foundation CoursePart Design Toolbars and IconsWorkbench IconBooleanOperationsSelection IconEnter SketcherIconAdvance Draft2. Dress-up Features –creates dress-up features onexisting geometry.3. Boolean Operations –used to Boolean Partbodies.Insert PartbodyIconReferenceElementsThere are eight maintoolbars within the PartDesign workbench: 1. Sketch based Features– creates geometric featuresfrom sketches.Sketch basedFeatures4. Reference Elements –creates 3D Points, Linesand Planes.5. Annotations – attachestext annotation to features.Annotation6. Constraints – createsconstraints on features.Constraints7. Transformations –applies transformationOperation to features.TransformationsDress-up FeatureCreation8. Surface basedFeatures – creates surfacebased Features.Surface BasedFeaturesThe Part DesignToolbars arealso accessiblevia the InsertDrop downDMS42184ANS-UG0300110Page 9 of 90Issue 1
AIRBUS UKCATIA V5 Foundation CourseThe Sketch Based Features ToolbarThis toolbar is used to create features from Sketches.Creates a PadCreates a PocketCreates a ShaftCreates a GrooveCreates a HoleCreates a RibCreates a SlotCreates a StiffenerCreates a LoftCreates a Removed LoftCreating PadsCreates different type Pad features by extruding a sketch profile linearly toproduce a solid.Creates aFilleted PadCreates multipledepth PadsCreates aPadCreates a pad from a Sketch to form a Solid feature by extruding a selectedprofile in a linear direction define by the user. If an solid geometry alreadyexists in the PartBody then the new pad feature will automatically added to it even iftit is not connected geometrically.DMS42184ANS-UG0300110Page 10 of 90Issue 1
AIRBUS UKCATIA V5 Foundation CourseSelect the Pad icon followed by the required sketch either graphically or from thespecification tree. If you have just exited a sketch then it will already be selected. APad Definition panel will now appear and a wireframe preview of the Pad bedisplayed. Enter a value in the Length field (default 20mm) or you can Grab theLIM1 and LIM2 text using MB1 to control the length of the Extrusion in twodirections and then dynamically drag the extrusion to its desired size. Now press OKto create the pad. The default is to create a pad exstruded distance normal to thesketch plane. The Reverse Direction and the Orange Arrow button swaps thedirection of the Limits.Dynamic limitText markers andReverse DirectionArrowCreated PadfeatureA Pad NodeThe Pad feature is added to the specification tree and the sketch that was used todefine it is now linked to the node.DMS42184ANS-UG0300110Page 11 of 90Issue 1
AIRBUS UKCATIA V5 Foundation CourseThere are various options available on the Pad Definition panel. By clicking on theMore tab the panel expands to reveal all the options.The following options are available: First and Second Limits control thelength of the extrusion about theselected sketch plane. The Type optionallows you specify whether theextrusion is a length or up to a surfaceor plane. The Length field is onlyavailable when Dimension is selectedin the Type field. The Limit field isavailable when up to a surface or planeis selected in the Type field.Profile/Surface allows you to specifythe sketch or surface that is used tocreate the pad. The Selection fieldindicate the sketch or surface that hasbeen selected. The Thick check box allows you the create a shelled extrusion byentering the thickness value in the Thin Pad fields.Mirrored extent if checked will deselect the Second Limit and create a pad extrudedequally about the sketch plane.As mentioned previously Reverse Direction flips the direction of the extrusion. Youcan also click on the orange Flip Arrow.Direction controls whether the extrusion is Normal to the profile or along aReference element.Thin Pad is used in conjuction with the Thick check box to create a shelled pad.Thickness 1 and 2 controls the thickness of the shell about the profile. If NeutralFiber is selected the shell is created equal about the profile and Thickness 2 isdeselected.The Preview button allows you to preview the pad.Clicking OK finshes the Command and creates the Pad Feature.DMS42184ANS-UG0300110Page 12 of 90Issue 1
AIRBUS UKCATIA V5 Foundation CourseThe following are examples of the different ways of creating a pad: If you select First Limit Type Up to surface the pad is extruded up to the selectedsurface.SelectedSurfaceSelectedProfileFlip ArrowResultingPadYou can create a pad up to but offset from the selected surface by entering a value inthe Offset: field.If First Limit Type Up to next is used the resulting pad will extrude up to the nextface of an existing feature. Up to Last will extrude up to the last face on an existingfeature.DMS42184ANS-UG0300110Page 13 of 90ResultingPad 1Issue
AIRBUS UKCATIA V5 Foundation CourseThe Thick option creates a pad with a thickness around the sketch profile rather thanjust a solid. The Neutral Fiber applies the Thickness 1 value equally about theprofile.ProfileCross sectionalthickness aboutthe profileThickness 1Thickness age 14 of 90Issue 1
AIRBUS UKCATIA V5 Foundation CourseIf Reference is select rather Normal to profile then the resulting pad is extrudedalong the select Line and not normal to the sketch plane.SelectedReferenceLineSelected Upto 00110Page 15 of 90Issue 1
AIRBUS UKCATIA V5 Foundation CourseHints and when creating PadsIt is possible to create a pad from a sketch that contains multiple profiles. Catia willautomatically select all profiles in the sketch and extrude them into a pad includingholes.Avoid creating multi profile sketches withopen profiles as this will result in Catiatrying to create open pads and failing.xWhen using Up to Next, Last and Surface the face or surface that the pad is beingextruded to must be large enough to fully intersect with the profile. This limitationdoes not apply to a Plane.When you use an entire Sketch to produce a Pad any elements contained within thesketch but not used in the profile must switched to Construction i.e. Points.DMS42184ANS-UG0300110Page 16 of 90Issue 1
AIRBUS UKCATIA V5 Foundation CourseWhen using a sketch with multiple profiles you can choose which of the profiles toinclude in the pad. After selecting the sketch to extrude thePad Definition panel will appear. Use MB3 on the Selectionfield to reveal a Go to profile definition pop up. Byselecting this option you can deselect profiles from within thesketch.A Profile Definition panel now appears which list the currentselection i.e. Sketch.1. Select Sketch.1 and click on theRemove button. The sketch is now removed from the list.Now click on the Add button and select therequired closed profiles or Sub-elements from thesketch followed by the OK button to create thedesired pad.Selected Profiles orSub-elementsDMS42184ANS-UG0300110Page 17 of 90Issue 1
AIRBUS UKCATIA V5 Foundation CourseCreates a Drafted Filleted Pad on an existing feature using a selected profile.Select the icon followed by the profile to be used to create the pad. The followingoptions are available: The Length is the length of the extrusion.The Second Limit must be selected and is usually the face of an existing feature onwhich the profile for the pad exists.The Draft applies a draft angle to the side faces of the pad. The Neutral elementeither First or Second limit controls which limit the draft angle is applied from i.e.the profile is at is original size.The Fillets options control the Lateral radius, First limit radius (the fillet nearestthe First limit) and the Second limit radius (the fillet nearest the Second limit).Reverse Direction reverses the direction of the pad.Clicking OK creates the feature.DMS42184ANS-UG0300110Page 18 of 90Issue 1
AIRBUS UKCATIA V5 Foundation CourseThe Specification Tree will now have a Pad created in ittogether with a Draft and three EdgeFillet features rather thanone all encompassing feature.Create multiple pads with different extrusion lengths.Select the sketch to use in the multi-pad command follow by the icon. A Multi-PadDefinition panel will now appear, use the More button to expand the panel to showall options.Use the First and Second Limit to definethe length of the extrusion. Note: Theonly option is a Dimension.The Direction option allows you extrudenormal to the sketch plane or along aReference Line.The Domains portion of the panel lists allthe profiles contained within the selectedsketch. By selecting one of the ExtrusionDomains, the values that are entered in theDimension fields control its length.Remember you can also Grab the LIM1and LIM2 graphically to control theextrusion length.Click the OK button to create the Pad.DMS42184ANS-UG0300110Page 19 of 90Issue 1
AIRBUS UKCATIA V5 Foundation CourseCreating a PocketCreates different Pocket features by extruding a sketch profile linearly tocreate a subtraction feature.DraftedFilleted PocketMulti-PocketPocketCreates a Pocket feature in a similar manner to creating a Pad.Select the sketch containing the pocketprofile and then select the icon. A PocketDefinition panel will now appear whichyou can select the More button to displayall options. The options on this panel areidentical to the Pad Definition panelexcept the resulting feature is subtractedfrom the previous feature in theSpecification Tree.The First and Second Limits control theDepth of the pocket about the selectedsketch plane. The Type option allows youspecify whether the extrusion is a depth orup to a surface or plane. The Depth field isonly available when Dimension is selectedin the Type field. The Limit field isavailable when up to a surface or plane isselected in the Type field.Profile/Surface allows you to specify thesketch or surface that is used to create thepocket. The Selection field indicates thesketch or surface that has been selected.The Thick check box allows you thecreate a thin pocket about the profile byentering the thickness value in the ThinPocket fields.DMS42184ANS-UG0300110Page 20 of 90InvertPocketArrowFlipArrowIssue 1
AIRBUS UKCATIA V5 Foundation CourseMirrored extent if checked will deselect the Second Limit and create a pocketextruded equally about the sketch plane.Reverse Direction flips the direction of the pocket or use the orange Flip Arrow.Direction controls whether the pocket is created Normal to the profile or along aReference element.Thin Pocket is used inconjuction with the Thick check box to create a narrow or thinpocket. Thickness 1 and 2 controls the width of the pocket about the profile. IfNeutral Fiber is selected the pocket is created equal about the profile and Thickness2 is deselected.There is an option to Invert the pocket by selected the second arrow that appearswhen the Pocket Definition panel is displayed. Note: This option does not appearon the panel. Click the OK button the finish.ThinStandardPocketsPocketsA Pocket node is added to the specification tree and thesketch that is used in its creation is added to it.InvertedPocketsNote: If you extrude the pocket in the wrong direction i.e. into open space andnot through an existing feature you will see a warning alert informing you thatthis operation is unnecessary unless the Pocket is in its own Partbody.DMS42184ANS-UG0300110Page 21 of 90Issue 1
AIRBUS UKCATIA V5 Foundation CourseCreates a Drafted Filleted Pocket.Select the sketch that is to be used to create the pocket followed by the icon. ADrafted Filleted Pocket Definition panel will now appear. The options are the sameas the Drafted Filleted Pad Definition panel.The First Limit is the Depth of the pocket.The Second Limit must be selected and is usuallythe face of an existing feature on which the profilefor the pocket exists.The Draft applies a draft angle to the side faces ofthe pocket. The Neutral element either First orSecond limit controls which limit the draft angle isapplied from i.e. the profile is at is original size.The Fillets options control the Lateral radius,First limit radius (the fillet nearest the First limit)and the Second limit radius (the fillet nearest theSecond limit).Reverse Direction reverses the direction of the pad.Clicking OK finishes the command.Again you can use the Invert Arrow to invert the pocket. eeResultingFilleting andDrafted PocketDMS42184ANS-UG0300110Page 22 of 90Issue 1
AIRBUS UKCATIA V5 Foundation CourseCreates multiple Pocket features with different depth.After selecting the sketch containing the pocket profiles and the icon a Multi-PocketDefinition panel will appear which is identical to the Multi-Pad Definition panel.Use the First and Second Limit todefine the depth of the pocket. Note:The only option is a Dimension.The Direction option allows you createthe pocket normal to the sketch plane oralong a Reference Line.The Domains portion of the panel listsall the profile contained within theselected sketch. By selecting one of theExtrusion Domains you can enter thevalue for the depth of the pocket in theDimension fields control its depth.Remember you can also Grab the LIM1and LIM2 graphically to control theextrusion length.Click the OK button to finish.Note: There is no invert pocket option for this command.Creating a ShaftCreates a revolved solid feature from a selected sketch profile.Select the sketch containing the profile followed by the Shaft icon. A ShaftDefinition panel will now appear containing the follow options: Limits defines the First (start) and Second (end) angles for therevolution of the profile. Default is a 360 revolution.Profile Selection field indicates which sketch you have select byusing MB1. Note: As with the Pad command by using MB3 onthe Selection field you can access the Go to Profile option andselect different profiles contained within the sketch.Axis allows you to define the axis of rotation. Note: You cancreate an Axis Line within the defining sketch and Catia willautomatically use it to produce the shaft.Click OK to create the Shaft.DMS42184ANS-UG0300110Page 23 of 90Issue 1
AIRBUS UKCATIA V5 Foundation CourseBelow is an example of a Shaft feature using a Profile sketch containing an AxisLine.WireframePreviewSketchDefiningProfileAxis LineResultingShaftfeatureDMS42184ANS-UG0300110Page 24 of 90Issue 1
AIRBUS UKCATIA V5 Foundation CourseNote: The Axis Line closes the profile and that the total Angle in the Limits cannot exceed 360 .A warning symbol will appear on the Shaft Definition panel if there is no Axisselected or if there isn’t one present in the sketch. A 3D Reference Line may be usedas an Axis Line.No Axis Selectedwarning symbolThe Specification Tree will have a Shaft node added to it and the defining sketch willbe linked to itCreating a rotational GrooveCreates a rotational Groove feature about an Axis Line.Select the sketch containing the groove profile followed by the Groove icon. aGroove Definition panel with the same options as the Shaft Definition panel: Limits defines the First (start) and Second (end) anglesfor the revolution of the profile.Profile Selection field indicates which sketch you haveselected. Again you can the Go to profile option to selectsub-profiles within the sketch.Axis defines the axis of rotation. Again you will see theno axis warning symbol if no axis is selected. Note: Byselecting an existing shaft feature Catia will use itsAxis as the Axis of rotation thus ensuringconcentricity between the Groove and the Shaftfeatures.Finally click the OK button to create the feature.DMS42184ANS-UG0300110Page 25 of 90Issue 1
AIRBUS UKCATIA V5 Foundation CourseBelow is an example of a Groove with an Axis Line defined in the sketch profile.Axis ooveFeature.A Groove node is added to theSpecification Tree with thedefining sketch attached.DMS42184ANS-UG0300110Page 26 of 90Issue 1
AIRBUS UKCATIA V5 Foundation CourseCreating a HoleCreates a hole in an existing feature without requiring a sketch profile.Select an entry face for the hole on an existing feature and then click on the Holeicon. A Hole Definition panel will now appear with three tabs along the topExtension, Type and Thread Definition.The Extension tab has the followingoptions: The hole limit tab allows to definewheather it is a Blind hole or that it iscontrolled Up to Last, Up to Next, Upto Plane or Up to Surface. The defaultis a Blind hole, which allows access tothe Depth field as well as the Diameter.If one of the other options is select thenyou have to select a Face, Plane orSurface to control the hole depth. Thereis also the option to Offset the depthfrom the selected element.Direction controls the direction of thehole into the feature. The Reverse tabreverses the depth (Note: If the direction is away from the feature i.e. into openspace, then a Hole node is created in the Specification Tree but there will be novisibility of a hole in the feature). The Normal to surface check box ensures thehole axis is normal to the entry surface, if this is unchecked you can select aReference Line as the direction of the Axis.The Positioning Sketch button allows you to enter a sketch to define the position ofthe hole on the entry face.The final option is the Bottom style for the hole, which is either Flat or V-Bottom,which allows you to enter an inclusive Angle.DMS42184ANS-UG0300110Page 27 of 90Issue 1
AIRBUS UKCATIA V5 Foundation CourseThe Type tab allows you to specify the type of hole that you require. The options areSimple, Tapered, Counterbored, Countersunk and Counterdrilled.The Parameter option allows you tocontrol the size of the hole featuresi.e. Counterbore size, depth of theCountersink, etc.The Anchor Point is only availablewhen you select either Counterboredor Counterdrilled and is used tocontrol the datum point on the hole inrelationship to the selected EntryFace.The Thread Definition tab can be used to assign thread attributes to the hole featurewhich can be extracted by other processes within Catia.After selecting the required options click OK to complete the feature creation.DMS42184ANS-UG0300110Page 28 of 90Issue 1
AIRBUS UKCATIA V5 Foundation CourseThe following are example of creating Hole features.A 10mm Diameter Blind hole.Selected Entry FaceWireframe PreviewSelect an Entry Faceand enter theDiameter value.Base Plate RadiusHole centre pointSelect the Positioningsketch button and apply aConcentricity Constraintbetween the Hole centrepoint and the base plateradius using MB3Click OK to createthe hole.DMS42184ANS-UG0300110Page 29 of 90Issue 1
AIRBUS UKCATIA V5 Foundation CourseA 10mm Diameter Hole with a 15mm Diameter Counterbore by 5mm deep.Wireframe PreviewSelected Entry FaceSelect the Entry Face. Enter the Diameter value andthen select the Type tab. Select the Counterboredoption and enter the Counterbore values.Select the Extreme Anchor Point to ensure the top ofthe Counterbore is positioned on the Entry Face.Select the Positioningsketch button on theExtension tab and apply aConcentricity Constraintbetween the Hole centrepoint and the base plateradius using MB3DMS42184ANS-UG0300110Page 30 of 90Issue 1
AIRBUS UKCATIA V5 Foundation CourseA quick way of constraining the hole centre to the base plate radius is to select theedge of the radius followed by the Insert Hole Icon and finally select the EntryFace. The hole centre will then automatically be constrained to the radius edge.You can also multi-select two edges to constrain to by holding down the Ctrl key andthen selecting the two edges before clicking on the icon. This will result in twoconstraints being created between the selected edges and the radius centre.DMS42184ANS-UG0300110Page 31 of 90Issue 1
AIRBUS UKCATIA V5 Foundation CourseCreating a Rib featureAllows you to extrude a profile along a reference element or pulling direction.Select the create rib icon. A Rib Definition panel will now appear. You have to selecta Profile and a Center curve. As with Pad creation you can useMB3 over the Profile field and select Go to profile definition toselect sub element profiles to create the Rib.Profile control defines how the Profile is extruded along theCenter curve: Keep angle is the default option and this ensures the Profile staysat the same angle to the Center curve as it is extruded. Pullingdirection keeps the profile parallel to a selected Line or Plane.Reference surface maintains a constant angle between the H Axisof the sketch profile and a selected surface.Merge ends will extrude the profile ends to join with an existing
AIRBUS UK CATIA V5 Foundation Course DMS42184 Page 4 of 90 Issue 1 ANS-UG0300110 Session 4 – The Part Design Workbench On completion of this session the trainee will: Be able to access the Part Design Workbench. Understand the Part Design Toolbars and Icon
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